HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

1. HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

Hi there I am wondering if anyone knows how to set the machine in metric?? G20 to G21 ?? ? ? I know that's Fanuc but does Okuma work like that too? or do you convert to inches?

I have done several threading jobs with this machine in inches however I am having a hard time writing Metric or converting it in Okuma

so basically I am trying to 9MM x 1.25 pitch

can anyone write a G71 line or tell me what to fill in the blanks in IGF?

major diameter 9mm
minor 7.647mm
pitch 1.25mm
TPI??
X Start .38"
X finish or minor diameter .301"
H[eight of thread]: .0266 I believe ? (or 9 - 7.647 /2 in MM)

that's all I got for now.

thanks

2. Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

Convert pitch to Imperial
1.25 / 25.4=0.0492

Calc TPI
1 / 0.0492=20.32

The lead is 0.0492'', the TPI is 20.32

Major dia = 0.354''

0.866 is a constant for metric thread depth
0.866*pitch = 0.866*1.25 = 1.0825mm = 0.0426'' thread depth
0.0426*2 = 0.0852''
0.354-0.0852=0.2687''

Minor dia = 0.2687''

This should give you enough to set it up just like cutting Imperial threads.

3. Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

Originally Posted by Jim Dawson
Convert pitch to Imperial
1.25 / 25.4=0.0492

Calc TPI
1 / 0.0492=20.32

The lead is 0.0492'', the TPI is 20.32

Major dia = 0.354''

0.866 is a constant for metric thread depth
0.866*pitch = 0.866*1.25 = 1.0825mm = 0.0426'' thread depth
0.0426*2 = 0.0852''
0.354-0.0852=0.2687''

Minor dia = 0.2687''

This should give you enough to set it up just like cutting Imperial threads.
thanks a lot, Jim. so provided all that
g50s200
T20202
G95
G97S100M3
G90G1X.38Z.1F50.
G71X.2687Z-1. H.0426 (D..005?) F.0492 (U.001?) M73M34
G80
yeah?

do you use M33 or M34? which is better? is it just preference?
I am putting threads on an already hardened 3/8" bolt. I bought a long one so I could cut it off and put threads on the end of it.

sorry if this is confusing

4. Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

is everything here radial ?? and no J value I take it since it's Metric ?or J is # of threads per inch
and we figured it's 20.33? does the machine like decimals?

5. Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

Does your machine have a G32 threading cycle available? That's what I use.

I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.

- - - Updated - - -

Does your machine have a G32 threading cycle available? That's what I use.

I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.

6. Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

Originally Posted by Jim Dawson
Does your machine have a G32 threading cycle available? That's what I use.

I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.

- - - Updated - - -

Does your machine have a G32 threading cycle available? That's what I use.

I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.
I think I tired it once but not G32
I tried G33 which is like G92 in faunc correct? I tried G33 but the control doesn't like it. so I have been working with G71 instead.
G33 X Z F J M23
X
X
X
..
seems pretty easy

but anyway where in IGF is M34 or M33 determined? and if you noticed in my picture spinning clockwise is written as M41 .. .
why?

7. Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

According to my list, the M41 is Spindle Gear Range 1, but I don't see a M3 (Spindle CW) or M4 (Spindle CCW) on your picture which is a bit odd. But understand I am no expert on Okuma or Fanuc for that matter. G33 (Fixed thread cutting cycle) by the description seems like a G32, but I'm not sure. In the example code below, the idea is to make a pass everytime a G32 is commanded, with a fadeout at the end of the thread. X and Z reposition at the start of the thread for each successive pass. Conversely, G71 combines this all into one line of code using a number of parameters. As near as I can tell, the M33/M34 tells the controller to fadeout the thread at the end (or not), not sure where this is invoked. Fusion 360 has a switch to fadeout or not.

This is a Haas turning post from Fusion 360, 9mm x 1.25 thread, 1 inch long converted to Imperial units. 5 passes with a spring pass. This will run on my lathe, but your lathe might choke on it. If you choose to try this be very careful, turn the feed and rapid way down.

N15 T100
N16 G99
N17 M22
N18 G97 S200 M3
N19 G54
N20 M8
N21 G0 X1.154 Z0.1969
N22 G1 Z0.246 F1.5748
N23 X0.3323
N24 G32 Z-0.9916 F0.0492
N25 X0.3491 Z-1. F0.0492
N26 G1 X1.154 F1.5748
N27 Z0.246
N28 X0.3155
N29 G32 Z-0.9832 F0.0492
N30 X0.3491 Z-1. F0.0492
N31 G1 X1.154 F1.5748
N32 Z0.246
N33 X0.2987
N34 G32 Z-0.9748 F0.0492
N35 X0.3491 Z-1. F0.0492
N36 G1 X1.154 F1.5748
N37 Z0.246
N38 X0.2819
N39 G32 Z-0.9664 F0.0492
N40 X0.3491 Z-1. F0.0492
N41 G1 X1.154 F1.5748
N42 Z0.246
N43 X0.2651
N44 G32 Z-0.958 F0.0492
N45 X0.3491 Z-1. F0.0492
N46 G1 X1.154 F1.5748
N47 Z0.246
N48 X0.2651
N49 G32 Z-0.958 F0.0492
N50 X0.3491 Z-1. F0.0492
N51 G1 X1.154 F1.5748
N52 Z0.1969

Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•